Beginner trying to learn basic programming

You need to break the shape down in to arcs and lines and also work out where you want the roughing passes to go.

I would suggest first either making an accurate scale drawing on paper or using CAD of both the required shape and the starting stock.
You can then draw note the critical points where arcs and lines intersect, and draw in your roughing passes as horizontal lines.

Doing this will also allow you to determine what tool geometry you need to make the part. (40 degree back angle, according to the drawing I just made in CAD).

You will find it easier to work in radius mode when hand coding arcs on a lathe. And you need to be in the XZ plane. You might prefer to use absolute arc-centre mode too.Then spindle speed and feed rate. I like CSS and feed-per revAll your G-code programs will start like this.

I suggest keeping this page to-hand:
linuxcnc.org/docs/2.7/html/gcode.html

Decide where your coordinate origin is. I like to use the -ve end of the material as zero, and that makes all y Z numbers negative.

Then measure the start and end positions of your roughing passes on your drawing, stopping slightly short of the profile. These form a sequence of rapid to start / feed move to end, feed out (or rapid out, rapid Z retract / Rapid X return / feed in moves.

Then program the finishing pass. If the sphere needs to be truly spherical then you need to compensate for nose-radius (G40 / G41) but initially it is easier not to.

Deciding where the arc finishes can be a little difficult if scaling from a hand drawing but you have chosen a convenient place for the arc end.
Note that lathe arc direction (clockwise / anticlockwise is as if you are lying on the floor looking up with a conventional front-toolpost lathe and as if looking down on a back toolpost
Then a retract to a safe place(G0 Xnn Znn) , spindle off (M5), coolant off (M9), end programme (M2)

This becomes much easier with G71 / G72 lathe macros, then you only need to programme the finish profile. There are ways to add that, and work is under way to do it as a built-in code.

Hand coding can let you do things that CAM never could. specially if you like maths and geometry:
bodgesoc.blogspot.com/2016/11/cams.html

My Arc Generator may help you sort out the arc portions of your G code.
github.com/LinuxCNC/simple-gcode-generators/tree/master/arcgen

My lathe subroutines may also help... I use these for 90% of my lathe ops.
gnipsel.com/files/chnc/subroutines/

JT

usert_l wrote:

The lathe I will be learning on is metric, not inches.

I wish you had said, I assumed inches from the drawing. I actually had to convert everything from metric to imperial, as I use metric pretty much exclusively.



I changed a few things, and got this.

I suggest you try the same thing, ie try running your code on the sim/axis/lathe simulator config to see your toolpaths.
I changed the negative X coordinates to be positive. (I don't think it matters with a lathe, but it seems an odd thing to do)
I changed the arcs to R format, because solving IK format from a hand drawing is difficult.
I changed the Z in G1 X-3.175 Z10 because that went straight through the ball....

I think it is actually waiting for spindle-at-speed.
Though why the sim would fail to reach speed is a mystery to me.

Try adding D5000 to the G96 line

It looks like the sim config tops out at 2500, so that is pretty much what you will see with small diameter work and a high surface speed.

You can edit the config, though bear in mind that this limit might not exist in the HAL of a real machine.

Have a look in the HAL at the "limit_speed" pins and parameters.
(And note that, because of what it is, maxv = acceleration, and max = max velocity)